Contour Milling - Siemens SINUMERIK 840D Operation/Programming Manual

3
Programming with ShopMill

3.5 Contour milling

Allowance (DR)
Example
3.5

Contour milling

Freely-definable
contours
3-186
You can program an allowance on the tool radius in this parameter
input field. A finishing allowance is then left when the contour is
machined (see also Sec. "Tools and tool offsets").
The DR parameter is active until a ShopMill cycle (drilling, missing,
contour missing) is programmed.
You want to leave a finishing allowance of 0.5 mm on a contour. DR
must then be programmed with 0.5 mm.
With a setting of DR=0, the programmed contour is cut without a
finishing allowance.
The "Contour milling" function is used when you want to mill simple
and complex contours. You can define open contours or closed
contours (pockets, islands, spigots) and machine them with path
milling or milling cycles.
A contour comprises separate contour elements, whereby at least two
and up to 250 elements result in a defined contour. You can also
program chamfers, radii or tangential transitions between the contour
elements.
The integrated contour calculator calculates the intersection points of
the individual contour elements taking into account the geometrical
relationships, which allows you to enter incompletely dimensioned
elements.
With contour milling, you must always program the geometry of the
contour before you program the technology.
You have the option of machining contours of any type by path milling,
stock removal from pockets with or without islands, or clearing
spigots.
The machining of freely-definable open or closed contours is generally
programmed as follows:
1. Enter contour
You build up the contour gradually from a series of different
contour elements.
2. Path milling (roughing)
The contour is machined taking into account various approach and
retract strategies.
3. Path milling (finishing)
If you programmed a finishing allowance for roughing, the contour
is machined again.
4. Path milling (chamfer)
If you have planned edge breaking, chamfer the workpiece with a
special tool.
SINUMERIK 840D/840Di/810D Operation/Programming ShopMill (BAS) – 10.04 Edition
3
10.04
 Siemens AG, 2004. All rights reserved